Tutorial: How to convert a .Step-File to an independent .CatPart-File in Catia V5

Kai

8 Jun, 2013 10:55 AM

This Tutorial shows you how to convert a .stp-file (dead solid) to an independent .catpart-file (iso-constrained) in Catia V5.
Using project/intersect 3D-Elements.

1. Step 1:

   -Open a new .CatPart-file in Catia
   -Open the .stp-file you want to convert
   -Copy the dead solid of the the .stp-file
   

   

2. Step 2:

   -Paste the dead solid in your new .CatPart-file
   (right click --> paste special --> as result)
   -Close the .stp-file
   

   

3. Step 3:

   -Change the color of the dead solid
   (right click --> properties --> graphic --> color)
   

   

4. Step 4:

   -Add a sketch on your CatPart and intersect the dead solid.
   (insert --> operation --> 3D geometry --> Intersect 3D elements)
   *Sketch support need to be a midplane of the dead solid*
   

   

5. Step 5:

   -Open the sketch analysis tool
   -Switch to "Use-edges" tab
   -Select the intersected geometry and isolate it

   *You can also isolate the geometry by selecting it --> right click --> selected objects --> isolate*
   

   

6. Step 6:

   -Get your sketch iso-constrained

   (You can use the "Sketch solving status tool" to check if your sketch is iso-constrained or under constrained)
   

   

7. Step 7:

   -Create a shaft of your sketch
   

   

8. Step 8:

   -Add a second sketch on top of the screw and select the lines of the screw head
   -Project the Lines from the dead solid into your sketch
   (insert --> operation --> 3D geometry --> project 3D elements)

   *Make sure to isolate the projected geometry prior you leave the sketch*
   

   

9. Step 9:

   -Create a pocket of your sketch

   

10. Step 10:

    The blue and grey shimmering surfaces are a sign that you have done all right.
    If you are not sure - switch the render style to "wireframe"
    (view --> render style --> wireframe)

    Now you can delete the dead solid and the work is done.